ShopBot Class Notes

From NYC Resistor Wiki
Jump to navigation Jump to search

The whole process is in n steps:

1) Design your thing.

You can do this using anything that makes vectors like Illustrator, Inkscape, or other drawing package. You may quickly find that this runs out of steam when you want to do very precise things or think more carefully about how things slot or fit together. You can also design right in V-Carve. For complex things, it really is worth the time investment to learn something substantial like AutoCAD, Fusion, QCAD, etc.

2) Turning your design into toolpaths

This is the part that demands the use of “CAM” - Computer Aided Manufacturing (contrast with CAD) - to turn vectors into toolpaths. Unlike the laser which conflates the two steps, using the ShopBot is much more like using a CNC mill or lathe (it really is just a huge CNC mill), which means the operator needs to think about what tool to use, where it’s going to go, and at what speed it’s going to spin and move.

3) Operating the machine itself, and cleaning up

This is the part where we move the toolpath into the ShopBot software, set up the machine and stock, run the machine safely, then tidy it up afterwards.

It’s worth noting that in a traditional machine shop these are often three separate disciplines and trades, many time performed by three different people or teams.

Step one: Design your thing[edit]

Designing an object is kind of beyond the scope of the course - this assumes that you’ve already come up with some sort of shape that you want to cut and have the vectors of those shapes outlined somewhere.

Step Two: Turn your design into toolpaths[edit]

This is where things probably get unfamilar. Here’s how this works.

As above, you have to choose, very broadly, three things:

  • The tool you want to use
  • How fast you want it to spin
  • Where you want it to go through the material
  • How fast you want it to go through the material

First, though, we also have to set up VCarve to know about the material we’re going to use.

  • Its X/Y dimensions (Vcarve only really knows about cuboid stock so if you have something that’s a funny shape you’re going to have to model it as a rectangle and make adjustments to your plan).
  • Its thickness, to a hundredth of an inch. Use a trustworthy caliper and take a few measurements at various points.s The nominal thickness of the stock isn’t really going to work - you really need real-world measurements.
  • Where the Z zero-reference is going to be. You have two choices: The top of the spoilboard/table surface (or, put another way, the base of your stock, or the top of your stock. Here are reasons for choosing one over the other.
    • If you’re going to be doing fine carving work where you are going to take pains to *avoid* going through the material, or if some of those carves are going to be shallow, then the top of the board is the best choice.
    • If you’re mostly going to do through-cuts where it’s important that you go through the material completely, then the bottom of the material is a better choice.
    • If you’re going to use more than one tool - that is to say, if your cut involves changing tools midway through, and you’re going to be using a whole shooet of stock that covers the entire table surface, then the top of the material is the best choice because that’s the most readily accessible surface to use as a zero reference. Remember that each time you change tools you have to re-zero the Z-axis.

Next, define toolpaths:

First, choose the kind of cut that you want to do. By far the two most common are profile (sometimes referred to as contour) and pocket.

Profile cuts are for cutting around stuff, or on lines. Useful for cutting things out, making grooves, and so on. Pocket cuts are for clearing areas. Useful for making holes in things and cutting out odd sized shapes and things where you don’t want to leave any waste-stock in the middle. Much slower than profile cutting.

For each toolpath you have to choose

  • The tool that you’re going to use.

Think about the edge finish you want and the size of the cut through you’re trying to make. An up-cut bit will force chips upward, giving you a smooth bottom edge but a rougher top edge. A down-cut bit will force chips down, giving a smooth top surface but a rougher bottom one, and will leave a packed lump of chips inside the cut (which is especially obvious with material like MDF which compresses into a pack). A straight-cut leaves chips sort of in-place and gives a smooth edge and slightly rough top and bottom finishes. Be very careful when using compression tools - they can make the chips extremely hot and require special handling - we don’t have any left out for general use.

Remember also that your tool is round, so if you want inside, angled cuts, they will have a radius equivalent to your tool. That can be fine, but if you want joints or tabs which slot together, you will have to fillet out the corners of the cut to allow the tab to fit in.

  • For a profile toolpath: the location of the cut - inside, outside or on. Think about what you want to end up with . Are you cutting a hole in something, are you cutting a part out of larger stock, or are you, say using a V-bit to get a groove that runs along a line? If you’re cutting something out, you want outside. if you’re cutting a hole, you want inside, and if you’re cutting a groove you probably want on.
  • Passes, depth, steps

When cutting through the material, either with a profile cut or with a pocket cut, you’ll want to set the cut depth to be slightly lower than the thickness of the wood - five hundredths to one tenth of an inch should be ample to cut through and not obliterate too much spoilboard. VCarve will give you some sensible defaults for the number of passes. A good rule of thumb when pocketing is that you don’t want to go through more than half the diameter of the cutter per pass.

  • Ramps

These are optimizations which make things nicer on the tool. Ramps are gentle step-downs into the workpiece. Most tools/endmills are not designed to plunge. That is, be pushed straight down into the material. It creates a lot of pressure on the end of it, which it isn’t designed to do; they are best suited for forward motion because that puts the most cutting surface against the material. The solution is a gradual descent into the material, called a ramp. You select over what distance the ramp occurs - the longer the distance, the gentler the slope of the ramp and the easier it is on the tool. However, you have to go over the area twice, essentially, so a very long ramp will lead to longer cutting time.

  • Milling direction

For wood, this isn’t terribly important. Conventional is fine, and easier on the tool. For metal, the shopbot is just about rigid enough to support climb milling if you’re trying to get very smooth edges. If you’re milling metal though, you probably didn’t need this document in the first place.

  • Tabs, etc

If you’re profile cutting out a bit of material, you’re presented with a problem: what to do with the stock that’s in the middle of the hole. If you do nothing, the stock will be left free with the cutting tool still touching it at the moment that the profile is completely cut, which will, at minimum, cause the part in the middle to wobble against the cutter, causing a big flaw in the edge. At worst, it will put a lot of stress on the cutter which might cause it to break and send fragments of cutter flying around the room. None of these scenarios are very good. Here are your options:

1) If the bit that’s going to be cut out is waste, you can screw it down to the table to hold it in place. This leaves the cleanest edge, but this comes with some constraints: The waste part has to be large enough to accommodate at least two screws to prevent twisting, and you must be very careful to measure where the screws are going to go relative to your toolpath - be sure that all the screws are away from where the tool is going to go.

2) You can leave a tiny bit of stock - a hundredth of an inch or less - holding the part in place which you then cut out and file off. This is called “onion skinning”. It’s tricky to get right and not recommended for a beginner because the tolerances involved are very tight.

3) You can leave tabs of material holding the part in place. This is the easiest, and well-supporetd by v-carve, and probably the safest.

  • Milling pattern

For pocket cuts, you can choose to either raster the shape that you’re going to cut out in scanline form, or go in circular format which roughly matches the outline of the shape you’re pocketing. It can be a little bit quicker to use a circular motion for rounder things.

Step 3: ShopBot operation[edit]

The checklist is the most important guide and should be considered authoritative. Here are some things we discussed as we went through:

  • Cleaning Collet

You can do this with compressed air, a gentle brush, or if it’s not dirty, just by knocking it on table to get the fine dust out of it.

  • Spoilboard clear of debris

Your cuts will be much more accurate with minimal stuff underneath the workpiece; the flatter the better. Be sure that there are minimal chips under the workpiece.

  • Zeroing the X/Y axis

There are two ways to do this; one is by using the built in X/Y zero to use the table’s own notion of its origin. This is good for repeatable work with whole stock of a known rectangular size. The other is by manually setting the X/Y zero to some other place. This can be better for stock which is of odd sizes that youve modelled in your toolpath as a rectangle. The latter is less accurate - a good optimization here would be to get a laser which fits into the collet.

  • Warming the spindle

This is done by - Going into ShopBot `full` mode (access from Easy mode via the ‘?’ menu) - Cuts -> spindle warmup routine

Ensure that the RPM monitor is open, otherwise the speed control won’t work. You can find that under ‘Tools’

  • Securing the workpiece to the bed

You have two options: - Screws Matt Borgatti has strong opinions. The idea is that you really don’t want to lift up the workpiece - you want to screw it down as much as possible, so strongly consider drilling pilot holes. Try not to use screws that will go all the way through the spoilboard. - Clamps Possible, but tricky. Also linear clamps probably just don’t have the clamping power you need, so use C-clamps if you can.

  • Zeroing the Z-axis

Recent events have encouraged us to disconnect the zeroing plate from the machine and stow it. This may not be really, truly necessary, but for now, plug it in, do your zeroing, and then remove it again.

  • Dust collection shoe

The dust collector is basically a giant vacuum - in order to be maximally effective, the shoe has to be touching the workpiece on its final pass. It shouldn’t be mashing against it, just brushing along the surface is fine.

  • Operator safety

Goggles on, earplugs in. Be near the E-Stops. There are three of them. 1) The soft stop which is operated by pressing the spacebar or clicking the ‘stop’ button. This will gracefully stop the current cut, move the spindle out of the workpiece, raise it to a safe Z height, and stop the spindle. It takes a few seconds 2) The button on the wall marked “soft stop” which does a very similar thing. 3) The big red button marked “Emergency Stop” which will cut the power to the machine. This is very hard ont it, but will really, truly, stop the machine cold. This should be used in case of fire, broken things, or other imminent danger.

Your order of preference is 1-3 above.

Tooltown doors are to stop any flying debris from exiting tooltown, and to prevent people from wandering in without wearing any safety gear. They aren’t there to keep you in.